+ Reply to Thread
Results 1 to 9 of 9

Thread: Loft Problem

  1. #1
    Senior Member Laurel's Avatar
    Using
    Inventor 2012
    Join Date
    Feb 2007
    Location
    Yorkshire, UK
    Posts
    138

    Default Loft Problem

    Hi.

    I'm having a bit of a problem creating a lofted feature. Please find attached the .ipt file in question.

    You will see a representation of a spool of tape following a path. You will notice a lofted feature which is supposed to show the tape twisting from one plane, through 90 degrees to another plane (think of it as twisting a roll of tissue paper as it is unrolled).

    As you can see (I hope), I can't get the tape to maintain its cross-section through-out the loft. I thought of using rails, but am not aware of a method of accurately drawing those in this case. I'd need to resort to guesswork.

    Any help would be very appreciated. Thanks.
    Attached Files
    Paul

  2. #2
    Senior Member Laurel's Avatar
    Using
    Inventor 2012
    Join Date
    Feb 2007
    Location
    Yorkshire, UK
    Posts
    138

    Default

    Ok, I've managed to make what I think is an ok job of the loft in question - please see the attached .ipt file.

    I created 4 3D Sketches and on each, drew a 3D spline which corresponded to a particular corner of the 2D sketches which would form the loft. These splines were then used as rails for the loft.

    I drew each spline starting from the edges which would form the ends of the loft, but doing this meant that the ends of the splines didn't flow smoothly in the directions I needed. To resolve this, I placed a tangential constraint between the spline and an appropriate edge at one end, and a similar constraint at the other between the spline and a 3D line I drew in the required direction.

    I have a couple of concerns about how I 'solved' this problem:

    1) Is it accurate?
    2) Is there a better and more accepted way to do it?
    3) I've never used 3D splines before, and those on this part are not fully constrained as I couldn't work out how to do so (a fixed constraint didn't seem to work). How do I resolve this?

    If anyone could offer any opinions, I'd be grateful.
    Attached Files
    Paul

  3. #3
    Forum Deity shift1313's Avatar
    Using
    not applicable
    Join Date
    Sep 2008
    Location
    VA
    Posts
    2,859

    Default

    my version of inventor is older so i cant open your files. Here is something i would probably do.

    what i did was draw a start/end rectangle to represent your paper cross section. It could just be a line if you were making a surface. I then drew a circle centered on one of the rectangles with the OD snapped to one of its endpoints. I then extruded this circle as a surface.

    In a 3d sketch i drew a straight line from one edge of the closest rectangle to the corresponding edge point on the far rectangle. Then i used project curve onto surface and used my cylinder to project it to.

    then i used sweep choosing one rectangle to sweep, my straight line between the two as my path and the projected curve as a guide rail.
    Attached Images
    Matt - Certified Solidworks Expert -Advanced Surfacing, Mold Tool and Sheet Metal Specialist
    Current Software: SolidWorks11,SolidCam11
    http://www.solidworkslessons.info/
    www.mysolidbox.com

  4. #4
    Forum Deity shift1313's Avatar
    Using
    not applicable
    Join Date
    Sep 2008
    Location
    VA
    Posts
    2,859

    Default

    I should also mention. if you can avoid using spline curves you will get a more accurate outcome for something like this. Also loft allows the object to transform between sketches. sweep wont allow this(besides a taper). Something like this where the tape(assuming it isnt pulled/stretched) is going to keep the same cross section through the transition would be better modeled with a sweep.
    Attached Images
    Matt - Certified Solidworks Expert -Advanced Surfacing, Mold Tool and Sheet Metal Specialist
    Current Software: SolidWorks11,SolidCam11
    http://www.solidworkslessons.info/
    www.mysolidbox.com

  5. #5
    Senior Member Laurel's Avatar
    Using
    Inventor 2012
    Join Date
    Feb 2007
    Location
    Yorkshire, UK
    Posts
    138

    Default

    That looks like a better way of doing it. The concern you raise about the loft method is exactly what I was thinking. I'll try your method. Thanks very much Shifty.
    Paul

  6. #6
    Forum Deity shift1313's Avatar
    Using
    not applicable
    Join Date
    Sep 2008
    Location
    VA
    Posts
    2,859

    Default

    cool. let me know if you have trouble/need more screen shots
    Matt - Certified Solidworks Expert -Advanced Surfacing, Mold Tool and Sheet Metal Specialist
    Current Software: SolidWorks11,SolidCam11
    http://www.solidworkslessons.info/
    www.mysolidbox.com

  7. #7
    Senior Member Laurel's Avatar
    Using
    Inventor 2012
    Join Date
    Feb 2007
    Location
    Yorkshire, UK
    Posts
    138

    Default

    Shifty (hope you don't mind me calling you that ) - I'm trying to perform the sweep as you described. It's easy to follow, and I understand it completely.

    Attached is a picture of my attempt. The dimensioned sketches at either end of the swept cylinder are the paper cross-sections.

    The example you described uses an extruded circle to make the cylinder. I swept mine along a spline which stretches from one cross-section to the other. This is because in my example, the cross-sections are not along the same axis. The spline can be seen in green, and is tangentially constrained to two straight lines (in black) at either end of the spline which ensures the path of the spline flows smoothly from each of the cross-sections.

    The straight line between corners is shown in black, and the projection in purple.

    When I try to sweep the cross-section along the spline using the path and guide-rail method, i get a 'modeling failure in ASM' error.

    Any idea where I am going wrong?
    Attached Images
    Paul

  8. #8
    Senior Member Laurel's Avatar
    Using
    Inventor 2012
    Join Date
    Feb 2007
    Location
    Yorkshire, UK
    Posts
    138

    Default

    Back again!!

    I don't know what the problem was exactly, but I managed to sort it.

    I did a little cleaning up - redrew the corner to corner line, deleted the tangent lines at the end of the spline path, recreated the surface cylinder and reprojected the projected line - and the sweep worked as required.

    Attached is a picture of the final result.

    Thanks very much for the help with a slightly complicated problem. I'm learning all the time with your help.
    Attached Images
    Paul

  9. #9
    Forum Deity shift1313's Avatar
    Using
    not applicable
    Join Date
    Sep 2008
    Location
    VA
    Posts
    2,859

    Default

    Registered forum members do not see this ad.

    paul it probably has to do with the fact that your cross sections are non planar. will it sweep just the straight path with no guide rail?

    the method i described probably wont work if the two end sketches are non planar.

    what you can do in this case is add another 3d sketch(or edit the one with your projected curve) and add another curve defining the "guide" for the other side as well. Then use the loft command. Becuase your guides are essentially constrained to that cylinder you should get no distortion of the loft.


    edit, i see you replied as i was. glad you got it sorted
    Matt - Certified Solidworks Expert -Advanced Surfacing, Mold Tool and Sheet Metal Specialist
    Current Software: SolidWorks11,SolidCam11
    http://www.solidworkslessons.info/
    www.mysolidbox.com

Similar Threads

  1. Trying to Loft a hook
    By Red_Stafford in forum Autodesk Inventor
    Replies: 81
    Last Post: 22nd Mar 2010, 11:53 pm
  2. Help with loft
    By MarvinX in forum AutoCAD 3D Modelling & Rendering
    Replies: 6
    Last Post: 4th Aug 2009, 02:59 pm
  3. Loft problem
    By Tomso in forum SolidWorks
    Replies: 13
    Last Post: 15th Apr 2009, 01:48 pm
  4. How can I fix this loft?
    By krautfed in forum Autodesk Inventor
    Replies: 25
    Last Post: 24th Feb 2009, 11:00 pm
  5. Loft
    By 270 in forum AutoCAD 3D Modelling & Rendering
    Replies: 4
    Last Post: 17th Jan 2008, 07:11 pm

Bookmarks

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts